Is there any guideline or rule for creating mesh like size of the grid depends on the minimum size of the geometrical model.

Hi!

This is a big topic.... but so fare, some hints:

regions with big gradients in the flow variables need a fine mesh. That means: where you have big changes in the velocity, temperature,... you need to have a dense mesh.

That is especially true for regions close to the wall. If you are interested in wall fluxes, your wall mesh should be fine enough, to resolve the boundary layer.

Here, it is necessary to take the wall functions into account. For some turbulence conditions, the boundary layer don't has to be resolved....

Another point is the mesh quality. The cells should not be to skewed, otherwise you will end up having numerical problems when simulating.

So.. its a big problem...

best wishes! Ralf

is there any rule that mesh size should be 1 tenth of the smallest element of the geometric model?

mhh.. difficult to say...

That rule may apply for the mesh close to the wall.

e.g. I had a cylinder in cross flow. The elements far away from that cylinder were in the same order of the diameter of the cylinder.

maybe you can describe your problem... and we can give some hints for meshing.

Ralf

i m modeling a earth tunnel heat exchanger in which a pipe is buried in ground for heat exchange between soil and the pipe. air is flown through the buried pipe. soil is acting as source and sink of heat for winter and summer respectively.pipe is buried about 3m depth in soil.

Hi Vikas.

You've raised an interesting, open-ended question: what makes a good mesh?

It depends.

It depends on your flow solver (Fluent, in this case) and what mesh metrics it's sensitive to.

It depends on the mesh type: hex versus tet versus...

It depends on what quantities you're trying to compute. Pressure? Temperature? Heat transfer? Terrible rules of thumb: to resolve the boundary layer and get good wall pressures your first cell needs to be at Y+ around 1. If you want heat transfer you need Y+ around 1/10. These numbers change, however, depending on the turbulence model, etc.

It depends on how long you want the solver to run. Got plenty of time? Throw several hundred million cells at it. Need something this afternoon? Try to be a bit more economical.

The answer is, there is no easy answer.

Hi John,

I just read your post and I am wondering about what you say about the yplus for best heat transfer simulation. It should be 1/10 - so you mean 0.1??

That is an extremely low value... were from do you get this? Is there any literature, that discusses that issue?

Another interesting point: The grow rate of the cells close to the walls has an effect as well. We found out, that there is a linear dependence between the HTC and the b/a ratio (a = first cell height, b = second cell hight).

Ralf

Ralf:

The Y+ = 0.1 number was dredged up from the dark recesses of my past in the days when I was involved in applied CFD for high speed flows.

You are absolutely correct that cell-to-cell size variation is important and most people like to keep that value below 2 (another rule of thumb) or even closer to 1.5.

Hi!

I even sometimes use a ratio below 1.2

It is just interesting, because we are doing some systematic investigations for some well known standard cases. What is the best mesh for right heat transfer simulation.

I never really found something in the literature about that...

Ralf

Ralf:

An even better trick, if you can afford to have a lot of cells, is to grow layers off the surface with a size ratio of 1 for several layers, then ramp up to 1.25, 1.5 etc.

If you don't mind my asking, what standard test cases are you using for your heat transfer simulations? If they are well documented (including geometry or CAD files, for obvious reasons), I'd like to look at them myself.

If I were to look in the literature for heat transfer simulations (and associated meshing requirements) I'd look for publications from the mid to late 1980s on hypersonic CFD.

Best regards.

John,

We do simulations with air at ambient conditions, turbulent, but incompressible.

Test cases were: the cylinder in cross and axial flow, the impinging jet, that plate in parallel flow and the wall mounted cube.

We are looking for local and integral heat transfer. One thing, that was really surprising: the available reference data does differ a lot!

For example the cylinder in cross flow: a student of mine does an intense literature research... and he came out, that reference values for integral heat transfer differ about plus-minus 40%!! (Re was between 4*10^4 and 1*10^5)

So far, nothing is published about that... But in a few month, i gonna finish my phd thesis about that... so you might get yourself a copy

Ralf

Ralf:

So my hypersonic experience does not apply!

One source of work you might want to investigate is research into the "personal micro environment". Researchers are studying heat transfer in and around a person in a built environment in order to perhaps improve HVAC systems. I know that Syracuse Univ. is doing a lot of work in this area in cooperation with a Danish (?) university.

which model i should use for evaporative cooling of air in a heat exchanger. how can i set the relative humidity of air coming to the H/E

[maddalena]

We are looking for local and integral heat transfer. One thing, that was really surprising: the available reference data does differ a lot!
...
So far, nothing is published about that... But in a few month, i gonna finish my phd thesis about that... so you might get yourself a copy

Ralf

Hi Ralf,
I am also wondering how to create a good mesh for heat transfer problems... (see http://www.cfd-online.com/Forums/mai...r-problem.html). May I get a copy of your thesis? It would be really useful for my purposes...
Thanks

mad